Siemens SINUMERIK 840D sl Function Manual page 61

The end point is deemed to have been programmed in the actual SAR block for approach if at
least one geometry axis is programmed on the machining plane (X or Y with G17). If only the
position of the axis perpendicular to the machining plane (Z with G17) is programmed in the
SAR block, this component is taken from the SAR block, but the position in the plane is taken
from the following block. In this case, an alarm is output if the axis perpendicular to the
machining plane is also programmed in the following block.
Example:
Program code
$TC_DP1[1,1]=120
$TC_DP6[1,1]=7
N10 G90 G0 X0 Y0 Z30 D1 T1
N20 X10
N30 G41 G147 DISCL=3 DISR=13 Z=0 F1000
N40 G1 X40 Y-10
N50 G1 X50
...
...
N30/N40 can be replaced by:
N30 G41 G147 DISCL=3 DISR=13 X40 Y-10 Z0 F1000
or:
N30 G41 G147 DISCL=3 DISR=13 F1000
N40 G1 X40 Y-10 Z0
Possible ways of programming the end point P
Tools
Function Manual, 06/2019, A5E47435126B AA
2.5 2D tool radius compensation
Comment
; Milling tool T1/D1
; Tool with 7mm radius
for retraction
0
W1: Tool offset
61